Hi there, I’m currently designing a ball bearing assembly but have run into an issue with the cage, I’m trying to make a cutout for the steel balls to snap into but fusion won’t let me cut how I need to and I can’t change cage dimensions, tried every workaround I could think of but to no avail so thought I’d ask smarter people lol.
A sketch should not have a single blue line in it before you do any Features.
I didnt watch this but Im sure its right based off the title
https://www.youtube.com/watch?v=iyc7urh8jhQ
a) Why did you revolve this, mirror it, and mess with Moves when you could've just drawn this all correctly in a single sketch? Arguably one of the worst ways possible of going about this. You never want to Move things (use joints) and you never want bodies to overlap (unless using a Join command after)
b) the file you attached already has a sphere cut out
@isaacfrazerb wrote:I’ve used as many constraints as I believed I need could you elaborate on what constraints I need in the sketch? Is that the issue?
Step 1 Start a new file and sketch a Rectangle at the Origin as shown below.
Crossing Window select the three lines to the right and hit x on the keyboard to toggle to Construction.
Select the vertical line from the origin and right click toggle to Centerline.
Add the dimensions shown below.
Observe the red padlock symbol on the sketch after adding the dimensions.
Now add a Horizontal Construction Line from the Midpoint of the Vertical Centerline over to the right past the Rectangle.
Add the dimension shown.
Observe the red padlock on the sketch after adding the dimension. (Click on the image below to enlarge the view.)
Now add a Circle at the end of the horizontal midpoint construction line.
Observe the red padlock symbol on the sketch glyph in the browser...
Now add a short vertical line in approximate location shown below.
Add the diametral dimension.
Add a Coincident Constraint between the top horizontal construction line of the rectangle and the top ENDPOINT of the short vertical line that we just created.
Observe missing red padlock symbol on sketch
Now sketch a short Horizontal line, and angle line and then a Vertical line (overtop of the construction line) as shown below...
Add the two dimensions shown below to constrain the angled line.
Observe the color change of the angled line after adding the dimensions (the actual color depends on your background color - might be different than my image).
Now add an angled line from the short vertical line down to the midpoint construction line.
Add the 45° dimension as shown below.
Now add a Tangent constraint between the 45° line and the Ø4.1 circle.
Observe the return of the red padlock symbol on the sketch (the sketch is once again fully defined).
Hopefully you anticipated the next step.
Add a Tangent Constraint between the vertical line and the circle.
Observe the red padlock symbol on the sketch.
Next go to the Surface tab and select Patch.
Click inside the boundary to create the patch (we will see why this technique in next step).
Attach your progress file here for next step.
